Shell and draft (or a different approach) for internal support for 3D print?

laird_broadfield

Deposition printing doesn't deal well with overhangs, so there are a several different approaches to supporting overhangs sufficiently to be printed.  


 Most slicing tools include semiautomatic generation of fill grids or breakaway supports.

 Some specialized tools are partly or all about support generation (Meshmixer shown):


 And some folks just design their part so there's no unsupported overhang -- this is the approach I'm wanting to find a recipe to easily accomplish.

(I've built a test document if anybody wants to play with this: https://cad.onshape.com/documents/f76d5c67855346c2aef32402/w/5f5fb53d0c6842ca93657284.)

Let's say this is my part; simple block with filletted top edges.



If I were making this for molding, I'd just shell it (maybe add some screw bosses and supports) then draft it.




But that big roof is really hard for a deposition printer to manage.



(For anybody who doesn't have direct experience, UT has a nice writeup and example pictures of things going badly here; scroll down to the "Limits of the 3D Printers" section.)

What I'm looking for is a simple recipe (just as, if I had molding in mind, shell-then-draft is pretty simple) for building support into the part.  In another tab of my doc is this...



...which I created by setting the thickest shell that still left any cavity at all, then experimenting with high draft angles until I got what looked like enough support.  

That process, however, is ugly and iterative, and once the part reaches real-world complexity, unworkable:



Without going all the way to a post-process with another purpose-specific tool (like Meshmixer) is there a simpler approach?  Some loft approach that's not obvious to me, etc?

julian_leland

@laird_broadfield: Here's what I usually do.

1. Create a sketch on the surface that I'm going to have contacting the print bed (in your case, the open side of your box)
2. Use the "Use" tool and other sketch tools to generate outlines for support structures. Typically, I do this by "Use"-ing all of the outer profile lines of the object being printed, offsetting them inwards by the minimum printable width that my printer supports, and then extruding them up to the object being printed. (Note to OS guys: In SolidWorks, I can save a step here by using the Thin-Extrude tool instead of offsetting & extruding. +1 for Thin-Extrude!)
3. If needed, I draft one of the faces of the supports outwards, so that the face where the extrude meets the build platform is thickest. This also makes sure that the edge of the support is thin where it meets the part, making it easy to remove.

Here's an image where you can see this being done - the two things I've indicated with blue arrows are support structures that I've added in.


In the specific case of your box, what I'd do is draw concentric boxes inside the hollow area of the box - probably spaced around 10 mm apart - and then extrude up to the inside of the box. Good luck!

julian_leland

@laird_broadfield: Here's what I usually do.

1. Create a sketch on the surface that I'm going to have contacting the print bed (in your case, the open side of your box)
2. Use the "Use" tool and other sketch tools to generate outlines for support structures. Typically, I do this by "Use"-ing all of the outer profile lines of the object being printed, offsetting them inwards by the minimum printable width that my printer supports, and then extruding them up to the object being printed. (Note to OS guys: In SolidWorks, I can save a step here by using the Thin-Extrude tool instead of offsetting & extruding. +1 for Thin-Extrude!)
3. If needed, I draft one of the faces of the supports outwards, so that the face where the extrude meets the build platform is thickest. This also makes sure that the edge of the support is thin where it meets the part, making it easy to remove.

Here's an image where you can see this being done - the two things I've indicated with blue arrows are support structures that I've added in.


In the specific case of your box, what I'd do is draw concentric boxes inside the hollow area of the box - probably spaced around 10 mm apart - and then extrude up to the inside of the box. Good luck!

laird_broadfield

julian_leland said:

@laird_broadfield: Here's what I usually do.
[...]In the specific case of your box, what I'd do is draw concentric boxes inside the hollow area of the box - probably spaced around 10 mm apart - and then extrude up to the inside of the box. Good luck!

That makes sense; I'd sortof had an inkling about selecting the baseplate outline of the void, offsetting in, and extruding up... maybe something like this:



That's not too bad, I suppose.

julian_leland

That will probably work. You may want to connect some of the support lines to the thicker walls, so that your printer doesn't break them off when they get tall but still haven't connected to the top of the box - it's a little harder to remove, but more robust to print. 

michael3424

Could the support structures be terminated just shy of intersection with the actual part, so by a layer height?  That might make separation easier of the support easier.  Someone on the Zortrax printer forum tried this a few months back and claimed to have success.

julian_leland

It's certainly possible to do that. My concern would be whether not having the bottom layer of your "roof" successfully adhere to a support would lead to it tearing off when the next layer is printed. That's part of the advantage of these contacting supports - they give the bottom layer of the "roof" something to bond to, which effectively creates shorter spans, which are more accurately located --> less likely to get torn by the printer. I haven't had too much trouble separating supports from my models when the supports actually make contact with the model: however, if you had a model where surface finish was extremely important, creating non-contacting supports (and probably increasing the number of supports as well) might be a useful tool.

mahmoud_2

@julian_leland
Very nice tip Julian. I design for my 3D printer all the time. I usually orient things to I don't use support, but that's a nice way to go about it. 

I think It'd be a good idea to offset the support structure by one layer height. So if you print at 0.1mm layer height, you can extrude your support and leave a 0.1mm gap so the top surface will dingle there for that 0.1mm but would still be supported in a way. 

christopher_owens

@julian_leland I like the tips on 3D Printing! I will be doing a lot of that. I my latest project I want to take separate Parts and create a Boolean to make the STL file. But I want to "Keep Tools" and save the Boolean as a "revision" or "version". Then I thought I would want the Boolean to be a "hollow dumb solid" and not modify if I update the parts. I've thought through a few ways to do this. But a "Keep Tools" and "Make Boolean/Part 'Stand Alone'"?? You also touched on support structures and I have thought of a "Hollow' part. I suppose a Boolean of a Scaled in Place Part inside a Part. Or Slice the Part in two, shell both pieces and Boolean back together. Perhaps under Shell could be a Hollow.

julian_leland

@christopher_owens - that sounds like an interesting (and complicated) project that you're working on.

In response to your first question, about using the Boolean to create an STL: Since there is no currently-available "Boolean Add + Keep Tools" option, I'd put the Boolean feature as the very last thing in your feature tree, and then roll back above it while you're doing design work. Then, when you're ready to print, roll forward past the Boolean, export the solid as a STL, and print!

Re: your second question - also interesting. I think it depends on the type of geometry that you're trying to create. If it's a simple shape - for example, a ball - either method will work. However, if it's a more complex shape - say, a coffee cup - then your first method (boolean of scaled part) may not work, depending on how the part scaling is performed. For instance, if the scaling function simulates all surfaces shrinking away an equal proportion from their walls, then your method will work fine. However, if the scaling function scales about a point (which I'm pretty sure it does), then it won't behave the way you want it to. In these situations, I'd go for splitting the part, shelling and adding, although you may occasionally run into weird geometry problems at the interface between the two shelled parts.

OS guys - I think there are two (good) feature requests here: Keep Tools addition to Boolean, and Scale Surfaces (or something like that - I don't know what the technical name for this would be)

Just to clarify (since I don't know how much 3D printing you've done), do your parts need to be hollow for design reasons - for example, you're modeling a water bottle - or are you just trying to reduce weight and save plastic?

andrew_troup

@Julian_leland :

Unless I misunderstand you, I think your requested "Scale Surfaces" is essentially "Thicken", which Onshape already features?

julian_leland

@andrew_troup - um - yes, that would actually be it. I thought that seemed like an obvious thing to include....Thanks for the correction!

christopher_owens

@andrew_troup , @julian_leland  Just to see if I could do it, I thought of creating a Support Part within a Hollow Part. The Hollow Part is a revolved Ellipse. The Support Part was created by sketching lines, using those to create surfaces, (which I notice you can't make a surface out of a "T"; the first surface was the horizontal line, then using one Extend-Surface operation to create surfaces out of all the vertical lines.) These were extended "both sides" a short distance.  A Thicken to make a Part-Support of the horizontal surface, and then a Thicken-Add to combine the vertical surfaces into the Part-Support. To get the surfaces to match the Ellipse's inside surface I did a few Replace Face while in a Section View. This allowed me to pick the faces of the Part-Support AND the inside surface of the Part-Hollow. Useful in the "real-world"?? Dunno!

billy2

I too miss thin extrudes also, but here's a work around for now.

Extrude a surface:


And then thicken the surface: